Y-axis lathe comparrisons

[YoDoug®]

I was at a customer the other day that has their erp system integrated throughout their whole process. They use bar code scanners attached to their lathes to generate macro variables for turning prehardened blanks. The intregration to the okuma osp control was just a simple vb script. The mazak and mori lathes cost tens of thousands of dollars and months to get the scanners working properly.

[Greg Williams]

The intregration to the okuma osp control was just a simple vb script.

 

The Windoze base does have some advantages. Below is a link to some info

 

http://www.okuma.com/thinc_magazine_issues/volume-02_number-01.pdf

[chris m]

And I could say your opinion is biased towords a certain product because thats what you use.

Do you have any other makes of Lathes?

 

Yes, we have Mori, Okuma-Howa, and Hardinge (barf) CNC lathes in addition to Okuma. Okuma makes the finest turning machines I have ever seen and the OSP control kicks Mitsubishi and Fanuc's a$$ in SO many ways; the fact that the iron and the electronics are made and serviced by the same company is a huge plus by itself. I think Mori makes some good equipment, but I think Okuma is better, and I deal with day to day operation of both for years after they clear the showroom floor.

 

C

[Joe788]

I was at a customer the other day that has their erp system integrated throughout their whole process. They use bar code scanners attached to their lathes to generate macro variables for turning prehardened blanks. The intregration to the okuma osp control was just a simple vb script. The mazak and mori lathes cost tens of thousands of dollars and months to get the scanners working properly.

 

Were the Mazak's over 10-12 years old? The integration for the Fusion or Matrix control should have been just as easy as the OSP.

[Joe788]

and the OSP control kicks Mitsubishi and Fanuc's a$$ in SO many ways;

 

LOL! In what ways would that be? (Specifically)

[chris m]

OK:

 

1) Assignment of my own local variable names

2) Alpha-numeric line numbering and subroutine naming ("NTURN" for start of turning called cycle, "NPROB" for start of probing cycle)

3) Easy use of logical operators and arithmetic functions without #501 this and #100 that

4) Blank shape definition for non-copy-turning canned cycles of premachined blanks or cast parts

5) Read current status of any machine input or output through the part program on (is load monitor on, single block on, op stop on)

6) Write to and read from tool length offsets or work offsets directly, no middle-man variables or G10 bullsh!t

7) Write to soft limits in machine for every tool or operation to prevent crashes or scrapped parts caused by offsetting errors or operator's pulse generator input

 

There's more but my fingers are tired

[Bruce Caulley]

Chris,

FYI 4,5,6 above can be done on a fanuc Oi series. I had a couple of lathes with the i-guide control and thought they were great. Not sure about the other things though.

 

Mori rep coming in today to compare.

 

Bruce

[chris m]

Wow my typing was bad in my last post, sorry for the somewhat Jenglish post guys. Bruce, that's good to know for Fanuc; I don't have experience with that specific control and may not be using the Fanucs I do have to their fullest extent because I find them to be SUCH a pain in the a$$. One of the guys who works for me is my Fanuc/Mitsubishi/Yaskawa control guy and I just keep my hand in enough to not be completely lost if he gets hit by a truck. Yaskawa had the best controls of that bunch from a user's perspective, hands down, and they don't make CNCs anymore; go figure.

 

I hope that you get some good info from the Mori people and feel like you have good facts to base your decision upon; I know from personal experience how much anxiety can be involved when laying down big capital on equipment knowing your name is etched across the machine in everyone's minds.

[Greg Williams]

FYI 4,5,6 above can be done on a fanuc Oi series.

 

What chris is saying is the status of ANY input to the PLC/Control can be checked from the NC program. This means any panel buttons ON/OFF status, Panel lights status, chip conveyer On/off, External M codes, etc etc. Also Any tool offset, wear offset, nose radius zero point or any other number can be set and/or checked from the Nc program.

[Bruce Caulley]

What chris is saying is the status of ANY input to the PLC/Control can be checked from the NC program. This means any panel buttons ON/OFF status, Panel lights status, chip conveyer On/off, External M codes, etc etc. Also Any tool offset, wear offset, nose radius zero point or any other number can be set and/or checked from the Nc program.

 

 

Ah, then only 4 applies

 

Bruce

[chris m]

That's exactly what I meant, Greg, thanks for translating

[Guest CNC Apps Guy 1]

1) Assignment of my own local variable names

SETVAR

3) Easy use of logical operators and arithmetic functions without #501 this and #100 that

See above

4) Blank shape definition for non-copy-turning canned cycles of premachined blanks or cast parts

Manual Guide i can do this... at least on a Nakamura-Tome it can.

5) Read current status of any machine input or output through the part program on (is load monitor on, single block on, op stop on)

Can be done.

6) Write to and read from tool length offsets or work offsets directly, no middle-man variables or G10 bullsh!t

Can be done

7) Write to soft limits in machine for every tool or operation to prevent crashes or scrapped parts caused by offsetting errors or operator's pulse generator input

Can be done.

 

So really we're only looking at ONE feature in your list ... #2... how appropriate.

 

That hardly qualifies as

...the OSP control kicks Mitsubishi and Fanuc's a$$ in SO many ways...

 

It's all in what you know. Just because I don't know whow to do something does not mean it cannot be done. FUnny... what I was a machinist, I thought I knew machines. Turns out I didn't know $#!+ !!! There's a whole other side of the machine that's there but it takes some knwledge, experience, and knowing the right people at your builder to exploit it.

 

Just sayin'

[Guest CNC Apps Guy 1]

After re-reading your list actually... the 30i series controls can partially do what you're asking. Line numbers AFAIK have to be line numbers, but sub calls can be alpha-numeric for ex.;

 

M98 <EATMYSHORTS> (NO spaces)

 

Can be called.

 

Program names can be just that, NAMES

 

%

<FANUC-RULES-OSP-DROOLS> (THAT IS MY PROGRAM NAME)

 

M30

%

 

JM2C

[Greg Williams]

I think we are comparing Okuma to Mori NL series so OSP to Mitsubishi, Can Mits do this?

[Guest CNC Apps Guy 1]

Ooops... typo... it is SETVN, not SETVAR.

 

To set the variable;

SETVN #501[FANUCV01] (LIMIT OF 8 ALPHA-NUMERIC CHARACTERS)

 

To call/use in a program, the syntax would be;

IF[#FANUCV01GT50]GOTO1001

 

 

I think we are comparing Okuma to Mori NL series so OSP to Mitsubishi, Can Mits do this?

 

I was responding to this;

...the OSP control kicks Mitsubishi and Fanuc's a$$ in SO many ways...

[GoetzInd]

Another thing to think about, there are a hell of a lot more people that run fanuc than anything else. At least around here there are. Makes finding a qualified operator and expertise a lot easier.

 

Mike

[chris m]

SETVN #501[FANUCV01]

 

This is still more complicated than TCUT=123456789; no initializing, no predefinitions, just BAM there it is

 

Sorry, man, Fanucs are powerful and do a good job of driving the machine but they suck to work with once you understand the power of the OSP User Task II

 

Does Fanuc have a canned bolt circle routine for machining centers yet? They didn't when we bought our last Fanuc-run VMC but that was awhile ago. Yasnac had one in 1985...

 

Mike, if both machines are absolutely equal I agree that would be a factor, but if they are not, it isn't in my opinion.

[Guest CNC Apps Guy 1]

SETVN #501[FANUCV01]

 

This is still more complicated than TCUT=123456789; no initializing, no predefinitions, just BAM there it is

 

Barely more complicated. Personally I still want to know what register I'm dealing with. There are already 30+ pages of

predefined WORD variables I can access including but not limited to tool offsets, work offsets, positions, etc... for example;

 

Tool Length Offsets for Offset 1;

Tool Length Offset Geometry

#_OFSHG[1]

Tool Length Offset Wear

#_OFSHW[1]

Tool Offset Radius/Diameter Geometry

#_OFSRG[1]

Tool LengthRadius/Diameter Wear

#_OFSRW[1]

 

Tool Length Offsets for Offset 199;

Tool Length Offset Geometry

#_OFSHG[199]

Tool Length Offset Wear

#_OFSHW[199]

Tool Offset Radius/Diameter Geometry

#_OFSRG[199]

Tool LengthRadius/Diameter Wear

#_OFSRW[199]

 

Does Fanuc have a canned bolt circle routine for machining centers yet?

 

You mean this;

 

%
O9010(B.C. MACRO OMC-32IM)
IF[#2EQ#0]GOTO100
IF[#11EQ#0]GOTO106 
IF[#24EQ#0]GOTO101 
IF[#25EQ#0]GOTO102 
IF[#26EQ#0]GOTO103 
IF[#7EQ#0]GOTO104
IF[#3GT1.0]GOTO105 
IF[#19GE#11]GOTO107
#100=#11 
#101=360./#100 
#102=#24 
#103=#25 
IF[#9NE#0]GOTO10 
#109=#4109 
#9=#109
N10#104=#2
#105=#7/2
#106=#3*10000
WHILE[#100NE0]DO1
#115=[#105*COS[#104]]
#116=[#105*SIN[#104]]
IF[#19GT0]GOTO15 
G0X[#102+#115]Y[#103+#116] 
G#106Z#26Q#17R#18F#9P#21 
N15IF[#19EQ0]GOTO16
#19=#19-1
N16#104=#104+#101
#100=#100-1
END1
G90G80G0 
GOTO108


N100#3000=1(START ANGLE  B MISSING) 
N101#3000=2(X-AXIS CENTER ARGUMENT MISSING)
N102#3000=3(Y-AXIS CENTER ARGUMENT MISSING)
N103#3000=4(Z-AXIS FINAL DEPTH MISSING)
N104#3000=5(BOLT CIRCLE DIA. MISSING)
N105#3000=6(C MUST BE PROG. WITH NO POINT) 
N106#3000=7(H=# OF HOLES,NOT ASSIGNED) 
N107#3000=8(SKIP AMOUNT TOO HIGH)
N108
M99
%

 

%
O0100 (BOLT CIRCLE CALL)
(CALL WITH CYCLE IN THE CALL)
G91 G28 G0 Z0
G90 G80 G49 G40 G0

G54.1 P1
G90 G0 X0 Y0 S1000 M3
G43 Z2. H1 
G65 P9010 X0 Y0 Z-.75 C81. H10. D5. A0 F20.
G80 M9
G91 G28 G0 Z0
M30
%

 

 

 

 

[Greg Williams]

Another thing to think about, there are a hell of a lot more people that run fanuc than anything else

 

That depends where you live. That may be the case in your neck of the woods, but it is not true for here. Also Mori NL's do not use Fanuc controls

 

[chris m]

James,

 

VTOFH[01] tool height offset for T01

VTOFD[01] tool diameter offset for T01

 

VZOFX[20] WOFS Z for WOFS 20

VZOFX[20] WOFS X for WOFS 20

VZOFY[20] WOFS Y for WOFS 20

 

VLMZB[08]=50 Load monitor base value for Z axis T08 = 50% thrust load

VLMZ1[08]=60 Load monitor #1 (worn out) value for Z axis T08 = 60% thrust load

VLMZ2[08]=65 Load monitor #2 (broken) value for Z axis T08 = 65% thrust load

 

You may not surrender, but you aren't going to claim victory either

 

Is that Fanuc macro one you wrote, or do they actually give one to customers now?

 

C

[Greg Williams]

James it is time to throw the towel in

 

(CHUCK OPEN DETECTION)

IF[VORD[1138] EQ 0]NALM1

 

(TAILSTOCK RETRACT)

IF[VORD[0064] EQ 0]NALM2

 

(SINGLE BLOCK OFF)

IF[VORD[0013] EQ 1]NALM3

 

(BLOCK DELETE OFF)

IF[VORD[0014] EQ 1]NALM4

 

(MACHINE LOCK OFF)

IF[VORD[0016] EQ 1]NALM5

 

(OPTIONAL STOP OFF)

IF[VORD[0017] EQ 1]NALM6

 

(COOLANT ON/OFF)

IF[VORD[095E] EQ 1]NALM7

IF[VORD[0030] EQ 1]NALM7

 

(LOAD MONITOR ON)

IF[VORD[095B] EQ 0] NALM8

 

(100% SPEED & FEED OVERRIDE)

IF[VORD[0022] EQ 0]NALM9

IF[VORD[0023] EQ 0]NALM9

IF[VORD[0110] EQ 0]NALM9

[Guest CNC Apps Guy 1]

Mori NL's do not use Fanuc controls

ACK!!!!!!!! Man... they sure are going downhill in a hurry. I always hated Mits controls.

 

You may not surrender, but you aren't going to claim victory either

FANUC Controls are a crapload more powerful than people give them credit for. The real problem is/has been that Mazatrol and OSP have PUSHED that stuff you're talking about whereas FANUC has had it for a LONG time but just never pushed it or talked about it. So because it's not pushed or talked about, people ASSume it does not have the capability to do that stuff and MANY of the people selling and supporting FANUC controlled products are ignorant as well.

 

Is that Fanuc macro one you wrote, or do they actually give one to customers now?

FANUC calls it CUSTOM MACRO B for a reason. What you do with it is up to you. I have probably a dozen or so Custom MACROs that I give to customers if they have or have the need, custom drill cycles, bold circles, spiral pockets, engraving, etc... It's part of Dealer Support. Oh, I did not write it. One of our other engineers did.

 

Greg, if a signal is issued to/by the control, I can read/check the condition of it, and depending on the function, control it as well form a program. Again, it comes down to the people supporting the machines and what they know or as in many of your cases... what they DON'T know.

[Bruce Caulley]

One of my mills had the i-guide and I think it had a bolt hole feature :headscratch:

 

As for operators, it is more common at the moment to find turners with mazatrol experience around here.

 

Bruce

[chris m]

I know why it's called CUSTOM macro B and we have many CUSTOM macros but not having canned bolt-hole-circles in your "world class" control is just another reason why people like me think Fanucs suck; I have canned bolt circles in my ProtoTRAK but not in my $200K machining center? Give me a break. Fanuc, like I said, makes powerful CNCs that do a very good job of driving the machine, they make extremely high-quality servo motors as well, but their programmer and operator friendliness sucks.

 

How about:

 

VCHIO=0 OD chucking

VCHIO=1 ID chucking

 

or

 

IF[VTOFZ[20] EQ 0]NALM1 TLO FOR T01 EQUALS ZERO

.

.

NALM1 VUACM[1]='TOUCH OFF TOOLS'

VDOUT[993]=9010

[Guest CNC Apps Guy 1]

Chris,

This discussion reminds me of the Mac vs. PC war. We're just going to have to agree to disagree. You're not going to change my mind about OSP and Mazatrol and I'm not going to change your mind about FANUC.

But, like I said before, all the things you listed so far are things I can EASILY do on many Nakamura Lathes.